Working with a String Object on a PCB in Altium NEXUS

Placed String objects

Summary

A string is a primitive design object. It places text on the selected layer in a variety of display styles and formats including popular barcoding standards. It can be user-defined text or a special type of string, referred to as a special string that can be used to display board or system information or the value of user-parameters on the board.

Availability

Strings are available for placement in both PCB and PCB Library Editors. Use one of the following methods to place a string:

• Choose Place » String from the main menus.
• Click the String button () in the drop-down on the Active Bar located at the top of the workspace. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar).
• Right-click in the workspace then choose the Place » String command from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter string placement mode. A string will appear floating on the cursor:

1. Position the cursor then click or press Enter to place a string.
2. Continue placing further strings or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

• Press the Tab key to pause the placement and access the Text mode of the Properties panel from where its properties can be changed on-the-fly. Click the workspace pause button overlay ( ) to resume placement.
• Press the Spacebar to rotate the string counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the PCB Editor – General page of the Preferences dialog.
• Press the X or Y keys to mirror the string along the X-axis or Y-axis.
• Press the L key to flip the string to the other side of the board.
• Press the + and - keys (on the numeric keypad) to cycle forward and backward through all visible layers in the design to change placement layer quickly.

Graphical Editing

This method of editing allows you to select a placed string object directly in the workspace and change its location, rotation, orientation or, in the case of inverted strings, size.

When a non-inverted string object is selected, the following editing handle is available:

A selected String (non-inverted)

• Click and drag B to rotate the string about point A.
• Click anywhere on the string away from any editing handles then drag to reposition it. The string will be held by point A and can be rotated (Spacebar/Shift+Spacebar) or mirrored (X or Y keys to mirror along the X-axis or Y-axis).

When an inverted string object with an editable bounding rectangle (inverted rectangle) is selected, the following editing handles are available:

A selected String (inverted and using an inverted rectangle)

• Click and drag B to rotate the string about point A.
• Click and drag C to resize the rectangle in the vertical and horizontal directions simultaneously.
• Click and drag D to resize the rectangle in the vertical and horizontal directions separately.
• Click anywhere on the string away from any editing handles and drag to reposition it. The string will be held by point A and can be rotated (Spacebar/Shift+Spacebar) or mirrored (X or Y keys to mirror along the X-axis or Y-axis).

The following methods of non-graphical editing are available:

Via the Properties Panel

Properties page: String Properties

The properties of a String can be edited in the PCB editor's Properties panel, which allows editing of all item(s) currently selected in the workspace.

During placement, the panel can be accessed by pressing the Tab key.

To access the properties of a placed String:

• Double-click on the String.
• Right-click on the String then select Properties from the context menu.
• If the Properties panel is already active, click once on the String to select it.

Editing Multiple Objects

The Properties panel supports editing multiple objects, where the property settings that are identical in all currently selected objects may be modified. When multiples of the same object type are selected manually, via the  Find Similar Objects dialog or through a Filter or List panel, a Properties panel field entry that is not shown as an asterisk (*) may be edited for all selected objects.

Editing via a List Panel

Panel pages: PCB List, PCBLIB List, PCB Filter

A List panel allows you to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the PCB Filter panel or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing you to target and edit multiple design objects with greater accuracy and efficiency.

Special Strings

While string objects can be used to place user-defined text on the current PCB layer, it is not only user-defined text that can be placed. To assist in producing documentation, the concept of special strings is used. These act as placeholders for design, system or project information that is to be displayed on the PCB at the time of output generation.

Examples of design, system, and design parameter special strings shown as source strings on the left and converted on the right.

The special strings that are available in a PCB document come from a number of sources:

• A default set of predefined special strings are provided for use with new PCB documents. A list of available special strings (system, design and available Project parameters) can be accessed in the Properties panel in Text mode, click the  button next to the Text editing box.
• Custom special strings can be added by defining additional parameters at the project-level – these parameters are defined on the Parameters tab of the Project Options dialog.
• User Parameters added to components in the Schematic domain are transferred via an ECO to become available to PCB components. If a special string that refers to a component parameter is added to a PCB footprint at the source library level, that string will be interpreted on the target mechanical layer or overlay when the PCB component is placed.

Notes about Using Special Strings

• If a string starts with the "." character, the entire string is treated as a 'special' string.
• To include more than one special string within a PCB string, enclose each special string within apostrophe ( ' ) characters; for example: '.Pcb_File_Name_No_Path' '.Print_Date'.
• You can also use text, spaces and special characters between concatenated special strings, for example: FileName= '.Pcb_File_Name_No_Path' : PrintDate = '.Print_Date'.
• Spaces and special characters can also be used within Project and Variant parameter names.

Placing a Special String

To use a special string on a PCB, place a string object then select one of the special string names from the  drop-down in the Properties panel. 

Accessing special strings for a placed string object.

PCB Predefined Special Strings

The following are the predefined, system-based special strings available for use on a PCB document:

• .Application_BuildNumber – the version of the software in which the PCB is currently loaded. When generating Gerber output, use this string to record the software build on which the design was created.
• .Arc_Count – the number of arcs on the PCB.
• .Comment – the comment string for a component (placed on any layer in the library editor as part of the component footprint).
• .Component_Count – the number of components on the PCB.
• .ComputerName – the name of the computer on which the software is installed and running.
• .Designator – the designator string for a component (placed on any layer in the library editor as part of the component footprint).
• .Fill_Count – the number of fills on the PCB.
• .Hole_Count – the number of drill holes on the PCB.
• .Item – the Item that the generated data relates to (e.g., D-810-2000). The data will be used to build that item.
• .ItemAndRevision – the item and specific revision of that Item that the generated data relates to in the format <Item ID>-<Revision ID> (e.g., D-810-2000-01.A.1). The data will be used to build that specific revision of that particular item.
• .ItemRevision – the specific revision of the Item that the generated data relates to (e.g., 01.A.1). The data is stored in that Item Revision within the target server.
• .ItemRevisionBase – the Base Level portion of an Item Revision's naming scheme (e.g., 1).
• .ItemRevisionLevel1 – the Level 1 portion of an Item Revision's naming scheme (e.g., A).
• .ItemRevisionLevel1AndBase – the Level 1 and Base Level portions of an Item Revision's naming scheme (e.g., A.1).
• .ItemRevisionLevel2 – the Level 2 portion of an Item Revision's naming scheme (e.g., 01).
• .ItemRevisionLevel2AndLevel1 – the Level 2 and Level 1 portions of an Item Revision's naming scheme (e.g., 01.A).
• .Layer_Name – the name of the layer on which the string is placed.
• .Legend – a symbol legend for mechanical drill plots. This string is only valid when placed on the Drill Drawing layer. Note: this is a legacy feature; place a Drill Table object for more detailed drill information.
• .Net_Count – the total number of different nets on the PCB.
• .Net_Names_On_Layer – the names of all nets on the specific layer. This string is only valid when placed on an internal plane layer.
• .Pad_Count – the number of pads on the PCB.
• .Pattern – the names of the component footprints used on the PCB.
• .Pcb_File_Name – the path and file name of the PCB document.
• .Pcb_File_Name_No_Path – the file name of the PCB document.
• .PCBConfigurationName – the name of the data set from which the output has been generated as defined in the Release view (Project Releaser).
• .Plot_File_Name – for generated Gerber output, this string identifies the file name of the Gerber plot file. For printed output, it identifies the layer depicted within the output. For ODB++ output, it identifies the name of the parent folder in which the files are stored.
• .Poly_Count – the number of polygons on the PCB (consisting of polygon pours, internal planes and split planes).
• .Print_Date – the date of printing/plotting.
• .Print_Scale – the printing/plot scale factor.
• .Print_Time – the time of printing/plotting.
• .Printout_Name – the name of the printout.
• .SlotHole_Count – the number of slotted holes on the PCB.
• .SquareHole_Count – the number of square holes on the PCB.
• .String_Count – the number of strings on the PCB.
• .Track_Count – the number of tracks on the PCB.
• .VariantName - the variant of the design from which the output has been created.
• .VersionControl_ProjFolderRevNumber – the current revision number of the project, which is incremented whenever a full commit of the project (i.e., including the project file) is performed. Version control must be used for this string to contain any information.
• .VersionControl_RevNumber – the current revision number of the document. Version control must be used for this string to contain any information.
• .Via_Count – the number of vias on the PCB.

Fonts and Barcodes

The PCB Editor uses TrueType fonts for string objects. In addition, support is available for presenting text strings in Barcode format. Barcodes are commonly used to tag and identify PCBs, streamlining inventory tracking through use of automated scan-machines, for example. Choice of font is made from the Text mode of the Properties panel.

TrueType Fonts

When using TrueType fonts, TrueType and OpenType (a superset of TrueType) fonts found in the \Windows\Fonts folder will be available for use. The feature also offers full Unicode support.

To use a TrueType font, set the Font Type (in the Properties panel) to TrueType then choose a font type from the drop-down field in the Font region. Use the B (bold) and/or I (Italic) options to add emphasis to the text as required.

Enable the Inverted option to display the text as inverted, with additional controls for the size, justification, and size of the border around the text.

Embedding TrueType Fonts

The PCB Editor – True Type Fonts page of the Preferences dialog provides options for embedding TrueType fonts when saving a design and for applying font substitution when loading a design. Embedding fonts is useful when text is required to be displayed in a font that may or may not be available on a target computer upon which the design is loaded. Font substitution enables specification of a TrueType font to be used as a replacement when loading a design where fonts have not been embedded and where fonts may not be available on the computer upon which the design is currently loaded.

The PCB Editor - True Type Fonts Preferences page

Stroke Fonts

Three Stroke-based fonts are available – Default, Sans Serif and Serif. The Default style is a simple vector font that supports pen plotting and vector photo-plotting. The Sans Serif and Serif  fonts are more complex and will slow down vector output generation, such as Gerber.

To use a Stroke-based font, enable the Stroke font option (in the Properties panel) and choose a font type from the drop-down field in the Font region.

Barcodes

The software provides the ability to place barcode symbols directly onto a PCB on any layer, allowing barcodes to be easily imprinted on a PCB as part of the manufacturing process. To use a Barcode font, set the Font Type field in the Properties panel to BarCode then define the display options as required.

BarCode ISO Code 39 (US Dept of Defense standard) and Code 128 (global trade identification standard) are supported and the actual text string from which the barcode is derived also can be displayed by enabling the Show Text option.

By using a combination of barcode and inverted text strings along with fills, if necessary, a clear barcode area can be defined on a board with more information textually than would otherwise be afforded by just the originating barcode text.

Example of using inverted barcode and additional inverted text strings.